Spindle Speed for tapping 1/4-20 holes.

[Loading]

Hi all,

I've got a Haas VF-1 with Rigid Tapping and I'm trying to tap some 1/4-20 holes. I have no idea what to use as a spindle speed. I guessed and chose 400 rpm, which gives me a feed of 20. I just broke the second one after a few holes. Any suggestions?

Also, I'm just spraying flood coolant during the tapping cycle. Should I manually be squirting rapid tap or something on the tap.

(I'm tapping them .55" deep)

Thanks!

[lakeside]

what material are you tapping? What type of tap are you using? is this a thru hole or blind? If it's blind try roll form

[Loading]

It is 6061-T6, it's a spiral flute. It's a thru hole.

Thanks!

[Ken_Shea]

You did not mention a lot of important factors to consider, so presuming aluminum 400rpm should not be a problem. I am a chicken when it comes to tapping, at least compared to post I have read, I use 200-250rpm for most everything I tap, but then I am not involved in production considerations, if it is deep I use rigid peck tapping and always take time to use tap-magic and blow out the chips between pecks.

I had a lot of problems using flood coolant and spiral taps, but did use a lot higher RPM then.

Yes it takes me a bit longer now but......No broken taps since.

EDIT, as Lakeside mentioned, form taps in aluminum are a real winner.
They take a different clearance hole so watch that.

[lakeside]

are you using a spot drill to put a chamfer lead in and are you use a two flute tap. I still like roll form

[Loading]

I'm not putting a chamfer lead in. Just spot drill it, then peck drill the hole.

It's a 3 flute tap.

I'm not worried about the speed, it's faster getting a nice tapped hole instead of breaking them.

I could switch to roll form. I'll need to figure out what clearance holes for em.

Thanks!

[Ken_Shea]

Loading,
If you end up trying form taps, here is a little tip, when spot drilling for the clearance drill go a little deep because the form tap will have rolled up a little mound at the hole entrance after tapping from the metal displacement.

[lakeside]

here some data on 1/4-20 roll form

[JPMach]

Check machinery's handbook for tap drill sizes for form taps. I highly recomend form taps or spiral point two flute tap for thru hole in aluminum. Alot of the other guys on here have great success with tapping around the speeds you said you tried, personally I tap 1/4-20 thru aluminum at 2500rpm and I haven't broke one yet. I've got around 110 holes on one form tap and it still looks as good as the day I bought it. I usually just have the flood coolant on but around every 20 holes or so I will coat the tap with a dry graphite film spray, I don't know that it does much after the first 1 or 2 holes but it can't hurt.

With form taps though just be sure you have the right size or a hair bigger hole drilled for the tap as a hair under will cause problems, I already coated one 5/16-18 tap with aluminum- not pretty. Also with form taps use a 90 deg spot drill and run it down far enough so that the tapped hole will be chamfered when all said and done, as the form tap displaces material, with no chf on top they will quite often roll material up above the top of the hole.

JP

[JPMach]

Lakeside, where did you get the neat chart program

JP

[Geof]

Tap drill 13/64", spiral point or spiral flute for through hole, 1000 rpm, 50.0ipm flood coolant. You should be able to do hundreds of holes with a single tap.

[Ken_Shea]

JP,
Since Mike is off wandering around other post.....

MEPro

It is the best $100 I ever spent.

http://www.cncci.com/products/cncmepro.htm